The Abaqus Interface for Moldflow reads the Moldflow interface files and creates the relevant files. The files created depend on which options you include on the command line when executing the Abaqus Interface for Moldflow. The files are described in the following sections:
For a midplane simulation the Abaqus Interface for Moldflow creates the following three files:
Partial Abaqus input (.inp) file
The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. It also contains a *STATIC step with default output requests. If you are working with isotropic materials, the input file contains material property data. Each input file begins with a series of comments that summarize the data provided by the Moldflow interface files and how the data are translated to the Abaqus input file. Additional data, such as boundary conditions and loads, and nondefault output requests must be added to this file manually.
Neutral (.shf) file containing material data for layered, spatially varying material properties
Material data are translated into an appropriately formatted ASCII neutral file. This file contains lamina material property data for each layer of each element. The Abaqus keywords *ELASTIC, TYPE=SHORT FIBER and *EXPANSION, TYPE=SHORT FIBER in the Abaqus input (.inp) file direct Abaqus/Standard to read material data from this file during the initialization step.
Data lines in the neutral (.shf) file:
First line:
Number of elements in the .shf file.
Number of layers in each shell section.
Subsequent lines:
Element label.
Layer identifier.
.
.
.
.
.
.
.
.
Fiber orientation angle (in degrees), measured relative to the default element orientation.
This data line is repeated as often as necessary to define the above parameters for different layers of a shell section within different elements.
Initial stress (.str) file
Residual stress data from the Moldflow analysis are translated into an appropriately formatted ASCII neutral file. These data are defined in terms of the local Abaqus coordinate system at each section point. The Abaqus keyword *INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS in the Abaqus input (.inp) file directs Abaqus/Standard to read initial stress data from this file during the initialization step.
If you are using an unfilled model, the Abaqus Interface for Moldflow creates only the partial Abaqus input file described below. For a three-dimensional solid simulation using a filled model, the Abaqus Interface for Moldflow may create additional files, as described below:
Partial Abaqus input (.inp) file
The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. Additional data, such as service loads and boundary conditions, and nondefault output requests must be added to this file manually.
Boundary condition data sufficient to remove rigid body modes are also included.
Material (.mpt) file containing orthotropic material properties data
Material data from the Moldflow analysis are collected and placed in a binary file. The data written to the file are in the same form as the information provided for the Abaqus keyword *ELASTIC, TYPE=ENGINEERING CONSTANTS. These are defined in terms of the local Abaqus coordinate system of each element.
Orientation (.opt) file containing element orientation data
Orientations defining the directions for material properties and initial stresses are computed and placed in this binary file.
Thermal expansion (.tpt) file containing element thermal expansion coefficient data
The orthotropic thermal expansion data from the Moldflow analysis are collected and placed in a binary file. These are defined in terms of the local Abaqus coordinate system of each element.